Guest EricFoy Posted June 15, 2013 Share Posted June 15, 2013 (edited) I have a model that is giving me incredible fits... The problem showed up as I was attempting to export in STEP format. The exported model would not import, except as a rather torn up surface model. Importing into Rhino revealed numerous "problem surfaces." Repairing manually in Rhino has proven *EXTREMELY* tedious and time consuming (partly due to my limited Rhino skills, I'm sure). But here's the deal. I have attempted to start over with the model, periodically exporting and re-importing to check model validity along the way, and it just always seems to blow up. In the past I have often "frozen" my models by exporting to .x_t or to .sat, then re-import. I did this to ensure that some smart feature didn't get out of order and ball up the works, and it always has seemed to work for me. This model, however just fails the acid test very early on in its development. It seems that perhaps the problem is a result of my fairly extensive use of variable-radius blends, but I don't know... Now I'm beginning to wonder if I don't have some kind of CPU bug -- like my machine is failing at edge trimming calculations or something. It doesn't seem to matter whether I'm using the Acis or Parasolid kernel, but I can't say I've done extensive testing in both. Is it possible that I need a new machine? Are the latest processors better at this stuff? Seems far fetched, but you never know... I know that a few years ago I had a model that would not regenerate, but when I put it on another PC, everything worked fine. Weird, but true. Or are there cumulative rounding errors going on that I can fix with a setting somewhere. Is there a setting for IronCAD's internal precision? Would it help if I modeled it at 10X scale, then scaled it down at the end? Scratching for answers. Edited June 15, 2013 by EricFoy Quote Link to comment Share on other sites More sharing options...
dprodanic Posted June 15, 2013 Share Posted June 15, 2013 Have you tried to do Combine shapes before export. Quote Link to comment Share on other sites More sharing options...
Jonas@Solidmakarna Posted June 17, 2013 Share Posted June 17, 2013 Hi Eric, In some cases with bad brep models exporting to IGES (as solid) and importing that file again can solve solid-to-surface issues. I guess the IGES format is to "dumb" to understand the tolerance issues and just makes a solid. Not always working but incredibly often. Your using Windows 7 Home, not "officially" supported. I don't think it is the issue in this case, but if you could try on a Windows 7 Professional/Ultimate (which probably also has another cpu) that might be worth trying out. As Dragan says you should also try the Combine Shapes tool under the Tools Ribbon tab (old UI under the Shape menu) which will combine all none suppressed features for the selected part into one brep shape (or the selected features into one shape). I would do that instead of exporting, then if it doesn't help export to IGES as solid and import again. Remember to make the import twice and switch to Parasolid/ACIS under the IC Options before importing the second time since the IGES file might be treated differently by the two kernels during import. I hope you'll find a way. Quote Link to comment Share on other sites More sharing options...
IronKevin Posted June 17, 2013 Share Posted June 17, 2013 Eric, If you'd like us to test it here, please send the file to support@ironcad.com or ftp://ftp.ironcad.us/incoming/ Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 17, 2013 Share Posted June 17, 2013 Another thing to try is to run the Statistics Check on the IRONCAD Model. This will tell you if there are problems before exporting. If there are some, you can attempt to correct them with some of the surfacing tools prior to export. The modeling tolerance of IRONCAD is at 10e-6. So if it is a solid without issues going out, it should come into most other programs as a solid without issues. Best Regards, Cary Quote Link to comment Share on other sites More sharing options...
David Thomas Posted June 18, 2013 Share Posted June 18, 2013 are you working within the same scene with all of this. I find quite often, copy and pasting my top level assembly into a new scene sorts out the gremlins. obviously you loose all your configurations... Nick Quote Link to comment Share on other sites More sharing options...
Jonas@Solidmakarna Posted June 18, 2013 Share Posted June 18, 2013 If the "scene container" (model geometry + all "other" ics file data) is the reason for the issue in some way you can always insert the ics file (no link) into a new ics file to remove old junk. Or "jump" to/from a catalog into a new scene. Kind of a purge function. Quote Link to comment Share on other sites More sharing options...
tcooksey Posted June 18, 2013 Share Posted June 18, 2013 I have a model that is giving me incredible fits... The problem showed up as I was attempting to export in STEP format. The exported model would not import, except as a rather torn up surface model. Importing into Rhino revealed numerous "problem surfaces." Repairing manually in Rhino has proven *EXTREMELY* tedious and time consuming (partly due to my limited Rhino skills, I'm sure). But here's the deal. I have attempted to start over with the model, periodically exporting and re-importing to check model validity along the way, and it just always seems to blow up. In the past I have often "frozen" my models by exporting to .x_t or to .sat, then re-import. I did this to ensure that some smart feature didn't get out of order and ball up the works, and it always has seemed to work for me. This model, however just fails the acid test very early on in its development. It seems that perhaps the problem is a result of my fairly extensive use of variable-radius blends, but I don't know... Now I'm beginning to wonder if I don't have some kind of CPU bug -- like my machine is failing at edge trimming calculations or something. It doesn't seem to matter whether I'm using the Acis or Parasolid kernel, but I can't say I've done extensive testing in both. Is it possible that I need a new machine? Are the latest processors better at this stuff? Seems far fetched, but you never know... I know that a few years ago I had a model that would not regenerate, but when I put it on another PC, everything worked fine. Weird, but true. Or are there cumulative rounding errors going on that I can fix with a setting somewhere. Is there a setting for IronCAD's internal precision? Would it help if I modeled it at 10X scale, then scaled it down at the end? Scratching for answers. 36167[/snapback] Eric, I had recently reported some problems I had with the step format. Models were similar to what you described ( torn up ) when imported into other packages such as Wildfire. Parts will be missing in the step file. This occurs when you have linked parts across different non linked assemblies. The first assembly it comes to will have the parts, but occurrences thereafter do not. So I am not sure that you can blame your machine. Seems like a problem with the Step translator or ICs integration with it. Troy Quote Link to comment Share on other sites More sharing options...
Guest EricFoy Posted June 19, 2013 Share Posted June 19, 2013 (edited) Yep. I've done all those things... Here's a reproduction of the problem I'm having. The real problem appears to center around the Shell operation. I think somehow that the shell, though it works great inside IC's internal works, fails to generate valid offset surfaces that can "stand on their own" when exported. I will test further, by generating offset surfaces manually, and then subtracting from the primary part to get the shell effect. But until then, I'd like it if someone else would try the following steps in order to verify whether I have a cpu problem, or whether it is a problem inherent with IronCAD... 1. Open the file, ICExportTrouble.ics 2. Export to STEP format 3. Import back into IronCAD, and see what comes in. Is it valid? Is it a solid? Or do you get, as I do, a shredded surface model? 4. If you can, import into Rhino, or another surface modelling program, and see what comes in... Here are the results I get: The original IronCAD file. ICExportTrouble.ics Here's what I get when I re-import into IronCAD Here's what Rhino produces. You can see that several of the internal surfaces are invalid, and one of the external surfaces is not properly trimmed. If I suppress the shell, then all the external surfaces seem to export and re-import just fine, so that is my current work-around. I will have to manually craft my internal shell subtractor to get the basic shape. Try exporting in either parasolid or acis format, and similar results ensue. UPDATE --------- Two more experiments: 1. If i select the outer surfaces, then CREATE|THICKEN to generate a shell model (in the downward direction), the resulting model exports and re-imports as a failed model, just as above. 2. If I create a second copy of the original [unshelled] model, then select all external surfaces and OFFSET them downward the thickness of the shell, then do a boolean subtraction of it from the original model -- Hooray. It works. This model re-imports just fine, both into IronCAD and into Rhino. Moral of the story: To create a robust model, don't trust the shell command. You must manually offset and subtract. *EDIT* : The above statement (regarding the shell command) appears to be be a false assumption based on a single unique experience. See my next reply below... Edited June 20, 2013 by EricFoy Quote Link to comment Share on other sites More sharing options...
Jonas@Solidmakarna Posted June 19, 2013 Share Posted June 19, 2013 It might be the combination of the Extrude Draft angle and the Shell. If I change the draft angle from 3 to 0 degrees and change the kernel to ACIS the STEP exp/imp works fine. Quote Link to comment Share on other sites More sharing options...
Jonas@Solidmakarna Posted June 19, 2013 Share Posted June 19, 2013 I replaced the Extrude Draft setting with a Draft Feature instead. It will work, but only using the ACIS kernel before exporting. ICExportTrouble_JB.ics Quote Link to comment Share on other sites More sharing options...
jolizon590016 Posted June 19, 2013 Share Posted June 19, 2013 (edited) Hi Eric, Tried your file and and attached the image of what I got. I tried combining the shapes before export but did not get it any better. I tried IGES and it gave better results. Regards, Joseph Edited June 19, 2013 by jolizon590016 Quote Link to comment Share on other sites More sharing options...
jolizon590016 Posted June 19, 2013 Share Posted June 19, 2013 Hi Eric, I tried the iges import options and now it it gave the 3D data. regards. Quote Link to comment Share on other sites More sharing options...
Guest EricFoy Posted June 20, 2013 Share Posted June 20, 2013 (edited) Well, after a bunch of further investigation, I have the following conclusion: My previous statement indicting the Shell Command as the culprit appears to be in error. The kernel appears to make a big difference here. What I have is a model with variable radius blends between curved surfaces, and it appears that the ACIS kernel is much better at handling these than is the Parasolid kernel. I've found that after performing a Surface Offset operation, the engine (both kernels) apparently continue to refer to the geometry as a surface generated by offsetting an original surface, who's geometry is retained for reference. I have deduced this by inspecting the contents of the exported Step file. This fact is further verified by the fact that importing some models into Rhino reveals misplaced surfaces - it brings in the original surface instead of the offset one. Importing into Rhino is useful for seeing "the truth" of what is actually in the Step file, since Rhino makes no attempt to solidify the part. IronCAD, on the other hand, kinda lies to us about what what's really in there, in a noble attempt to maintain the part's supposed solidness. Unfortunately, IronCAD is really good at doing this, so when an import into another application is attempted, said application might not be able to stitch it like IronCAD can. And this is the source of my problem... Anyway, I've found that by careful monitoring, and *especially* by using the ACIS kernel, I am able to maintain model integrity. This has been a fascinating, though bothersome adventure. But thanks, IronCAD, for providing us BOTH KERNELS to work with! Edited June 20, 2013 by EricFoy Quote Link to comment Share on other sites More sharing options...
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